I am trying to nest 24" base cabinet sides on a sheet of 94"x97" melamine. If I outline with a 3/8" bit and set an additional part clearance of 0.04" (to clear joinery on adjoining pieces) the controller wont nest two deep in the Y direction. Does anyone currently get the controller to cut two 24" parts wide on a standard sheet of melamine? Please share your tricks and tips, I need to get the control nesting to do this. The e-cabs nester will do it but my controller seems to prefer not to. The jobs we are currently doing are 50-60 cabs per job and the off-fall really adds up at the end of a job; too many to handle efficiently.

First off, you should not have to add any "Additional Part Clearance" as Control Nesting should be augmenting the gap between parts automatically based on a preset ratio.

Also, you should make sure that you do NOT have a "Collar" value set. (This field should in fact read "Additional Collar".) Control Nesting automatically calculates a default "collar" based on the Outline Tool diameter (approx. 50%) unless "Nest to Edge of Sheet" is selected.

As long as you are not adding EXTRA clearance anywhere, you should be able to nest the two 24" gables in the 49" wide material.

I have the collar set to 0. I'll try to attach a picture of the completed sheet nest on the table. I'm cutting a full width dado for the deck and top that ends flush with the back of the cabinet using a half inch downcut. The diameter of the bit forces the end of the cut past the edge of the piece. I'll have to check the ecabs file and make sure there is no abnormal inset to the end of that dado. That is the only thing I can think of that might be wrong.

On a side note, as you can see in the picture, when outlining with the compression bit the kerf is filled with dust that the collector doesn't suck out. This would obviously make it difficult for the bit to stay at optimum operating temperature and directly affects tool life. I'm pushing this bit (an AMANA mortise compression, 3/8") at 720 in/min and at 18000 rmp. it is a two flute and it gets so hot I cant touch it after cutting parts out of one sheet. I have gotten about 4 hours out of these bits before they are smoked. They are literally black. Do you think I should speed this up or slow it down to try to increase cutting life, or is this about right as far as expectations for bits used to outline? What are you using, if you outline with 3/8", and what are your feeds and speeds. Been wondering if PCD is worth the extra cost, and can run at the same speed. TIA to everyone!

A lot of operators, saying good things about Vortex Bits, especially cutting melamine. Another suggestion is, can you try another brand of sheet material? That could make a big differenceCheck out woodweb.com this is a popular topic

A non-mortised tool is going to clean out way better. Your speeds all look good but the chips are not getting removed fast enough causing them to recut. The extra heat will wear your tool faster causing even more heat.

Forrest

As a side note, I've tried the 2 and 300$ dollar diamond bits with very little success. The best tools so far are the Vortex XP series although they are a little more pricey. You should be able to cut at least 100 sheets of 3/4" melamine with this tool. And after that keep cutting plywood with it because the main wear will be where the paper surface contacts the bit leaving a chip in the edge.

Forrest Chapman wrote:A non-mortised tool is going to clean out way better. Your speeds all look good but the chips are not getting removed fast enough causing them to recut. The extra heat will wear your tool faster causing even more heat.

Forrest

As a side note, I've tried the 2 and 300$ dollar diamond bits with very little success. The best tools so far are the Vortex XP series although they are a little more pricey. You should be able to cut at least 100 sheets of 3/4" melamine with this tool. And after that keep cutting plywood with it because the main wear will be where the paper surface contacts the bit leaving a chip in the edge.

Good to know those PCD bits aren't a real value, that would be a tough pill to swallow.

I use a downcut bit for the dados and I've recently switched back to the non-mortise bits for outlining. My bit still gets super hot and the kerf is still full of chips. I wonder just how much more suction the dust collector needs to provide, or if there is some other causal link I am missing.

As to the dado overcut showing on other pieces, I have some negative insets at the end of the dado to make sure the cut clears the workpiece and doesn't mess up the joinery on the part, -0.25 for the 1/2 diameter bit I am using. I'm stumped as to how to solve this problem other than completely changing the joinery method or trying to dado with a smaller bit. If I use a 0.375" Diameter bit, each dado is going to need three passes, right? seems like this would add substantial cut time to jobs.